I am still struggeling with the problems mentioned in this post:

http://www.cfd-online.com/Forum/cfx.cgi?read=14887

I thought I would ask instead if anyone has sucessfully applied the Gamma-Theta Transition model, and if so under what conditions and with what mesh?

I am thinking maybe the weirdness I am seeing is due to the structured mesh or something, even though it shouldn't matter in theory...

/C

Hi, I am using the Langtry Menter transition model on a simulation of a first stage turbine blade with low inlet turbulence intensity (0.2 %)and I am having the same problem that you described (transition location skipping around every grid point). Actually, I did a previous simulation with a higher level on inlet turbulence intensity (about 4%) and I was not getting this strange result, even though the transition location was predicted earlier compared to the experimental data I have. I am trying to figure out where the problem is. I followed the guidelines that are suggested in the manual (yplus <1, number of nodes in the streamwise direction). The only thing that I can tell you is that the first time I ran the simulation with low turbulence intensity I was not applying any initial condition and after some iterations I would get a linear solver failure on the mass conservation equation. If I looked at the results I would not get a transition at all. So what I did was run a laminar simulation with the same boundary conditions and use the results from that as initial conditions for my sst simulation with the transition model activated. The results of this simulation are the ones that have the jumping transition issue. I would really like to solve the problem so I am very willing to share any information about the matter. If you have any questions I'll gladly answer so maybe with the effort of two people we'll come up to something.

Francesco

Try refining the grid in the streamwise direction around the transition zone. The "spikes" usually occur when there arn't enough streamwise nodes to resolve the transition zone (which can occur over a very short distance relative to chord, particularly when the boundary layer is close to separating).

Robin

Thank you for the suggestion. I will try to refine the mesh in the streamwise direction and will post the results. I would like to ask a couple of questions to you about the transition model.

I am simulating a linear turbine blade cascade. I am trying to match the turbulence conditions I have in the wind tunnel experiment I am running. The turbulence in the windtunnel is generated with a vertical bar grid. I am running a separate boundary layer simulation to obtain the boundary layer profile to apply at the inlet of the cascade simulation but I am having some trouble fixing the inlet conditions for this preliminary simulation. I have different possibilities in CFX (Turbulence intensity and length scale, turbulence intensity and viscosity ratio). I have information on the experimental turbulence intensity so that's easy to match but I don't have an exact idea of what to use as length scale or viscosity ratio. I tried different length scales (a dimension comparable with the dimension of the bars, a higher dimension, a lower one). I am pretty confused with the results because up to the transition point all the simulations have quite similar results but what happens is that the transition location moves depending on the value of the turbulence length scale at the inlet. Is the transition mainly sensible to the inlet turbulence intensity or should the turbulent length scale also play an important role? Another this is that I read this sentence on the CFX manual that I did not quite understand:

"It has been observed that the turbulence intensity at the inlet can decay quite rapidly depending on the inlet viscosity ratio (cut) ... If the viscosity ratio is too large the skin friction can deviate significantly from the laminar value. (cut) At this point it is not clear how accurately the transition model reproduces this behaviour. For this reason, it is desirable to have relatively low (i.e. 1-10) inlet viscosity ratio and to estimate the inlet value of turbulence intensity such that at the leading edge of the blade the turbulence intensity has decayed to the desired value".

With the length scales values I used as inlet conditions for the boundary layer simulation, downstream of the inlet I obtain viscosity ratios that are much higher than 10 (in some regions 400). Does this mean the transition model will not produce accurate results? Should I set the viscosity ratio instead of the length scale at the inlet of the boundary layer simulation?

I would really appreciate having answers to these questions and I feel that you would be the best person to receive this information from since you collaborated in developing the transition model.

Thank you very much and sorry for the very long post.

Francesco

Hi Francesco,

the problem you are having is not specific to modeling transition.

If you have a uniform inlet velocity profile and no walls or other obstructions in the inlet region and are using a standard 2 equation or even RSM turbulence model, the model will give no production of turbulent kinetic energy since there are no gradients.

When you set the boundary conditions at the inlet, whether it is intensity and length scale or viscosity ratio what you really are setting is the inlet condition for k and epsilon. The relations between length scale and eps usually look something like eps = k^1.5/L_t

Then what you have is some level of k at the inlet, no production but a non-zero dissipation.

What makes this worse is that various levels of intensity, length scale (or equivalently epsilon or eddy viscosity ratio) with different inlet lengths can give the same k and epsilon just upstream of the body, blade, wing, etc....that is very bad!

For consistiency with the above problem a lot of folks have taken to making eddy viscosity ratio at the inlet = 1.0

Write out the relations by hand and convince yourself of this if you are still confused.

Hope this helps,

Bak_Flow

Well, from what I can see refining the grid in the streamwise direction does not seem to change much. I have tried now with 250 streamwise nodes, which is about as far as I can realistically go given my computer resources. (Mesh is about 5M elements in total)

Boundary layer: y+ = 1 (on the laminar parts), 20 layers, expansion 1.3. This simulation was left to run _way_ passed the point where all variables were converged to make shure there were no such problems.

Still see the same effect.

Fransesco, I was thinking about the influence of inlet turbulence you talked about, since I am running with very low settings here too (the foil is actually under water, so turbulence is very low). I wanted to do a simulation with higher inlet turulence and maybe use the correlation coefficients to account for that. Maybe not correct, but just as an experiment to see if the numerical problem would go away. But I cannot find anything in the documentation on the meaning or use of the coefficients...

http://img65.imageshack.us/img65/567...anscfx34gi.jpg

Hi again,

I ran another simulation with 4% turbulence intensity at the inlet. I started it from a well converged laminar solution of the problem. Unfortunately I got the transition issue this time. I did 150 iterations and I noticed the following things.

1) At a certain point (iteration n 40 -70) the residuals start having fluctuations (in particular the energy equation residual). After iteration 70 the fluctuations stop and the residuals go down smoothly but quite slowly. The Rethetat equation instead starts having small fluctuations from iteration 80 and keeps on staying that way.

2)The intermit equation does not converge well. I get RMS residuals around 10^-3 and max residual 10^-1. Does the intermit equation converge well in your case??

3)I have some results saved at iteration 18, 100 and 128. At iteration 18 I get transition on a large part of the suction surface of the blade, but no "jumping" transition. At 100 the transition moves downstream but the transition issue appears. At iteration 128 the "jumping issue" becomes much more evident. Unfortunately I don't have results files between 18 and 100. Do you have a chance to look at intermediate results files on your simulation?

What are the correlation coefficients you mentioned in your post about increased turbulence intensity??

Regards Francesco

The model has some "correlation coefficients" (I believe they are called CI1 CI2 etc, don't have access to the software right now).

The manual says that they can be used by the user to tune the correlation model, I presume to match experimental results. But the manual is silent as to how they are defined and supposed to be used...

Based on your statement that the "jumping issue" did not appear for higher inlet turbulences I was thinking (just to get an idea whats going on, not necessarily get accurate results) to increase inlet turbulence and then tweak the coefficients to get a correct transition point.

However if you still see the jumping issue at 4%, then this doesn't sound like it would give anything...

An expansion ratio of 1.3 is actually pretty high for a laminar/transitional boundary layer. In certain cases it can mean you only have 5 - 10 nodes in the laminar boundary layer which may not be enough to resolve it (and the transition process) correctly. Try bringing the expansion ratio down to something like 1.1 or 1.15 and see if this helps at all. Also if this mesh was made in ICEM Hexa you should set the Tri tolerance to a small value (0.0000001) as it can effect how accurately the mesh is projected to the geometry and can show up as "spikes" in the wall shear.

Robin Langtry

Interesting. Reason for using 1.3 expansion was trying to accomodate the boundary layer on other parts of the model where it grows quite thick. I am trying 30 layers @ 1.15 expansion now (and the tri tolerance decrease) to see if it solves the issue.

Your input is much appreciated! /C

Well, not having much success...

I try here to provide as much info as possible so maybe my mistake can be spotted!

This simulation uses 30 layers at 1.15 expansion, y+=1 for the areas of the foil with low turbulence, up to y+ about 3 - 3.5 for the more turbulent areas. An ICEM Tri tolerance set to 1e-7. I am not using ICEM Hexa, but a mix of hexa in the boundary layer and Tri's throughout the rest of the volume.

The spikes are still very much present.

If I look at the Transition Onset Reynolds number outside of the boundary layer, the results look reasonable, indicating an immediate transition on the lower side of the foil and an area close to the expected results on the upper.

Also the Transition Reynolds Number does not exhibit the spikes very much. Here you see a plane between spikes:

http://img81.imageshack.us/img81/772...anscfx45di.jpg

And here is one on a spike:

http://img139.imageshack.us/img139/3...anscfx60le.jpg

For reference, this is what the convergence behaviour looks like for 100 iterations (Mom/Mass, Turbulence and Transition):

http://img66.imageshack.us/img66/587...anscfx57bb.jpg

Also for reference, here are the relevant parts of the input file to make shure there is nothing funny with the settings:

FLOW:

DOMAIN: Domain 1

Coord Frame = Coord 0

Domain Type = Fluid

Fluids List = Water ...

BOUNDARY: In

Boundary Type = INLET

Location = IN

BOUNDARY CONDITIONS:

FLOW REGIME:

Option = Subsonic

END

MASS AND MOMENTUM:

Normal Speed = 5.14 [m s^-1]

Option = Normal Speed

END

TURBULENCE:

Eddy Viscosity Ratio = 1

Fractional Intensity = 0.0005

Option = Intensity and Eddy Viscosity Ratio

END

END

END ...

DOMAIN MODELS:

BUOYANCY MODEL:

Option = Non Buoyant

END

DOMAIN MOTION:

Option = Stationary

END

REFERENCE PRESSURE:

Reference Pressure = 1 [atm]

END

END

FLUID MODELS: ...

TURBULENCE MODEL:

Option = SST

TRANSITIONAL TURBULENCE:

Option = Gamma Theta Model

TRANSITION ONSET CORRELATION:

Option = Langtry Menter

END

END

END

TURBULENT WALL FUNCTIONS:

Option = Automatic

END

END

Hi, I have much better results, but I have no idea, how I can import a picture.

PetrK

Well that's a lot easier that running CFX, so you should be able to handle it :-D !

Create the image on your local disk, go to www.imageshack.us, browse for your local file, press "Host it!", and from the resulting page cut and paste the "Hotlink for websites"-field into your forum message.

If you publish some results, it would be interesting to know as much info as you can provide on you settings, mesh data, fluid models, inlet conditions and so on!

/C

Hi,

Even though you say you have the recommended near wall spacing, it appears you have a big jump in mesh sizes from that up to the surrounding tet mesh. Have you tried extending the inflation layers beyond the boundary layer so the jump in mesh sizes is further away from the boundary layer?

Also, have you done a 2D model of this? In 2D you should be able to have a far more detailed mesh again and that would be a good one to exploe exactly how fine a mesh you need for the 3D model.

Regards, Glenn

Hi PetrK,

I would be grateful if you could post some information on your mesh, settings and initial conditions because I am having the same problem Chebeba is having and I haven't solved it yet.

Thanks, Francesco

See my results in the new topic : Has anyone successfully used transition modell..p2